(Question) Selective insert changing

[randy5061]

Im currently working on some A36 Steel and im facing it down to size and iv noticed after my roughing passes when i want to finish and i check the tool only 3 out of the 6 incerts on the 2" face mill are worn.  What would be some the pros and cons to only changing out the the worn incerts and leaving the ones that had no vissable chipping or wear?

[gcode]

I would check your facing tool and spindle for runout.

Something is not right. 

[crazy^millman]

Tells me that cutter is not good and needs to be replaced if new then send it back as defective. Each insert should be at the same place. Use an indicator and check there positions. If they are not within .0005" of each other then try to readjust them if they will not then it supports the cutter is no good.

[gcode]

Also, take the face mill off the arbor and make sure the mating surfaces are spotless and there are no

dents or debris that may cause Z axis runout.

[SlaveCam]

As others have hinted, here are no pros. You'll get a broken cutter body in no time. Changing inserts is an all-or-nothing operation. Only for tools where cutting speed varies between inserts, such as indexable drills, where the outer insert tend to wear more rapidly, it makes sense, but even then you need to control tool life for both inserts somehow.

If your inserts are being worn unevenly, are you mixing different grades?

[huskermcdoogle]

Another thing to note when you have some inserts that are worn and others that don't appear to be.  Runout is certainly the normal cause.  Fix that and the problem will be less apparent.  But I find usually it is also a sign that you don't have the right cutting parameters.  If you are taking enough chip load and are going fast enough to not get built up edge a few thousands of runout won't cause you any harm.  But if going too slow, some inserts may be failing early due to built up edge ripping the coating off the inserts.  This will appear randomly as wear on some inserts but not on others especially on easy to machine softer steels like A36.  Otherwise, too little feed will rub on some and cut on others as the difference in chip load due to runout will put you on the other side of not enough feed.  Feed 25% harder and it might go away.  If it doesn't, check the speed.  If it were me...  In A36, I would be running a CVD coated insert @1200+ SFM and about .010"ipt as a starting point.

 

Unless you have ground inserts, .0005" runout axially or radially is asking for a bit much.  For standard pressed inserts in a milling cutter .0015-.002 isn't abnormal, especially in the 3-5" range.  If the inserts are clocked the same way they were pressed, .001 should be achievable, but you may have to play with swapping inserts and pockets around, or custom clocking the inserts to fine adjust, especially if there is a little mileage on the cutter.  For ground periphery sub .001, should be pretty easy as long as everything is clean, and the body and mounting is in good shape.  If your screws are worn, replace them, so you can get consistent torque.  Better yet torque your screws, and plan to replace screws on a regular basis.